Printable View
This 2010 screen-set is nothing short of brilliant!
A couple of questions...
Workflow, does this seem correct?
Mount the work,
Mount Tool 1,
Set X&Y zero position,
Run initial auto zero,
Cut job.
Probing...
What is needed in order to use the X&Y probing routines - what is the 'probe'?
Tools...
If tool 2 is longer than tool 1, will it hit the fixed probe plate?
i.e do we need to try and get the tools similar in stick-out?
Not tried this yet - just looking to learn.
Thanks
The "probe" is usually the tool. Actually, to use the screenset as is, it needs to be the tool.
Make sure that you set the Clearance Plane to a high enough value so that all tools will clear the plates, and buy a safe margin. There's some info on this in the 2010 manual.
Keep in mind that the maximum probing distance is coded at 150mm (assuming you're using metric). If you need more, I can tell you how to change it.
Ok, I will increase my clearance plane, manual only advises 3mm i think above fixed plate - thats what made me ask:)
The probe i am asking about is the one used when running the X & Y probing wizards - if the tool is grounded and the work (being metal) is grounded it cannot work, one needs to be isolated? Also the sides of an end-mill would not be accurate enough to probe an edge with?
I think 150mm is fine as thats all the Z i have.
I thought you meant for the Z axis tool length probing. For that, you need to use the tool, and use an isolated plate.
Yeah I got that working perfectly, very slick ;)
It was the edge wizards I was interested in now.
Then you need to use a real probe.
ok, thanks, will do some searching.
If your probing to an edge, you can use an isolated plate along the edge and specify the plate thickness. Then just use a precision dowel to probe with.
Interesting idea, thanks.
Back to my OP, still working out the niggles...
Where i am roughing with the 5mm tool, i have 2.5mm rads in all the internal corners, the finish tool of 2mm will plough into these at full speed - recipe for breakage here ??
Where we sorted the three slots out on the left with the roughing passes on the small tool, would it be better to pre-finish pass the whole part with the 2mm tool to bring the corners down to 1mm rads+finish allowance and then run once round with the finish pass at full depth??
This would mean i get rid of the fiddly pre-finish op on the three slots as they will come under the new full pre-finish runs. These runs would be contouring at 0.6mm DOC per pass.
I recall JAZZ mentioning it should be ok on page 1 but having seen a 2mm tool now, it seems a heavy cut on the full height of the tool??
Attachment 17993
The green section plus the portion from the base of the 5mm circle etc. plus an extra 0.1mm finish allowance (not shown)
Well first you'll finish at lower feed than roughing and because of the Rad the stress on the 2mm tool is progrssive with the highest stress being fraction of the cut.Quote:
Originally Posted by Davek0974
Give it big blast of lube/air when entering corner and it will fine.
Oh well, not there yet:upset:
I spent a while assembling a fogless coolant thingy, plans as found all over the 'net, pretty easy build, seemed ok.
This was my setup - pre-drilled the cut-to-size plates so i had a fixed position, jig style setup.
Attachment 18018
First run was at FS calc speeds, new 5mm high helix carbide tool, that ended up in a right mess very rapidly, boy did it complain! The fact that it managed to carry on ripping through the metal with a fully loaded tool was quite impressive - tough little some-bitch this machine!
The tool did not break!
After the "what the f*** was that?" moment passed I hit the e-stop! On examining the aftermath, it appears the new coolant system stopped the coolant and was just on air only, this allowed the tool to load up and that was the end.
After an hour of messing i got most of the gunk off the cutter - that stuff was welded up!
Attachment 18019
Upon removing the plate from machine I could see the carnage below, the load-up had pulled the tool from the collet and happily chewed my nice new bed:upset:
Attachment 18020
I cleaned that up with a flat file and tried again. Same cutter but this time I altered the parameters from one ramped full depth roughing pass to stepped multiple passes of 0.81mm at 1500mm/min.
I also cranked up the coolant but it sucks big time and is the typical fogger system that i did not want - the whole room filled with oil/paraffin mist, I can still taste it! Totally unsuitable but i pressed on as i did not want to be beaten on this.
I got a video of it roughing out - https://youtu.be/A9ZqR9chMwg
Things seemed a bit happier, fingers were crossed.
Then came final pass on the 2mm tool - again nice new solid carbide, the small holes were run at 1000mm/min at 0.62 DOC, ramped - these worked perfectly and i was impressed here.
The pre-finish on the three loops at the bottom again worked perfectly.
The final pass on the outside edges was at full-depth and 0.1mm cut, 1000mm/min - this is where it all fell apart again - the corners of the cutouts where the larger rads were left made a bit of a squeal but first cuts worked ok, the left side of the main part cut ok on one side of one notch but the second broke the tool and that was it for the day.:miserable:
Attachment 18021
I had ordered spare cutters but some were crap and had to go back, that left me with just one 5mm and one 2mm from another supplier - the 2mm is trash and the 5mm is still gummy after about 1mm depth.
The final part is above - onion skinning will not work as there is a slight variation in bed heights and the part cannot be removed fully. I think tabbing and a sacrificial sheet of hard card or something under the plate will work better.
I also have an odd issue where mach3 went into reset when on the line before a tool-change - it would stop the spindle, lift up to clearance height then sit there in reset, pressing reset again allowed the spindle to come to park position for tool-change and then carried on normally. This happened a few times. My only suggestion here is interference from the M05 spindle-stop triggering the reset and this stopping the code right before the M06 command. I have a filter for the VFD and will bung that in.
So, unless I can find some tooling in the Bridgeport cabinet, I'm stuffed for the weekend.
I also need a coolant system as paraffin mist must be bad for health, it certainly tastes like crap!
It's easy done when you start cnc machining (and from time to time when you've been doing it a while)
You need to get used to the machine and dial it in accordingly. You'll get there
I've been machining a number of parts recently and have supported the work piece using parallels (on their side) to lift it slightly off the bed. Then pushed a piece of thin MDF under the work to reduce the vibration. The parallels keep the work flat relative to the bed and you can cut at least 1.0mm through to make sure it is free without hitting the bed. I used tabs to hold it.
Just before each pass (when it is ramping down) I vacuum around the profile to clear the previous chips and give a bit of WD40 spray and repeat until done. I don't have a compressor so this is my way currently
Good luck with the fog buster development as I think that is a good long term approach
I'm not getting any more tooling from eBay, just ordered some 2mm and 5mm single-flute carbide tools, more swarf clearance and a stiffer tool, from Cutwell - part E5E47020 was one of them. Recommended for Aluminium and plastics.
The previous eBay ones I ordered three 2mm high helix 6mm flute, I got one that was 5mm long and two others of a random length and unknown but obviously wrong helix angle, they refunded them but it left me short on cutters.
Hopefully I can find some tooling in the cupboard to get me going again of the weekend.
As for the coolant, i'm going to drill out the jet from 0.6 to 1mm and try that - it should lower the air velocity and increase droplet size hopefully.
There is one other remote possibility - Aluminium warehouse have goofed up again and sent a soft grade of alu when I wanted 6082 T651, they have done this once before and i spent a weekend trying to figure out what was wrong with the plasma cutter when all it needed was the correct aluminium. :(
I will switch to tabbing as well, can't be any worse ;)
Been digging through the cutter drawer, found loads of 3mm carbide 3 flutes, some 4.5mm and 5mm 3 flute cobalts as well plus a 2.5mm cobalt.
I isolated some of the features on my part and run them in the scrap from yesterday - i hate wasting metal ;)
I also tweaked the F & S sliders in HSMAdvisor to suit my machine rpm and also a lower feed-rate (i had not done this yesterday so it was running full production rates :concern: or at least trying).
Using the 5mm 3-flute and a 3mm 3-flute, plus the modified coolant (much better with nozzle cut off) I set some different paths and all seemed ok, 1mm DOC was quite happy on the 5mm with 30% step-over
on the pockets, the 3mm was ramped down to a full 5mm cut at 0.1mm deep and that seemed ok too, the end result...
Attachment 18033
4 perfectly cut features. I even got a bit of video.. https://youtu.be/uIuylK4Y7qs
Annoying bit is that I can't try cutting a real job as the job is designed for 2mm finish tooling and it fails in CAM if i try using the 2.5mm cutter so I will have to wait until new cutters arrive now.
I think the single flutes will do well - lots of chip clearance and slower feeds. I have also re-cammed the job for full cut + 0.05mm and added some tabs, it will be cut on a 0.3mm spacer sheet.
Educational....
As i have ordered some cutters from a reputable supplier now, I asked them what the recommended cut specs were for rpm, chip load and feed. They instantly sent me a nice chart with it all on, feeding the data into HSMAdvisor shows up where i was probably going wrong a bit :)
Things alter rapidly when you give the calculator the correct data - i was running too fast, too deep, too much chip. Adjusted specs for a 2mm single-flute carbide would be...
18,000rpm
2.5mm DOC
600mm/min feed
I recall when i snapped the 2mm on the weekend I had it set at something like 1400mm feed and 5mm DOC :)
Helps having correct data i guess.
Wow! This sh1t gets expensive fast ;)
This sorry saga relates to the part shown in the OP.
Waited a week for the cutters to arrive, first 5mm carbide bit the dust in 30 seconds! The speed calculated at 12000rpm and using my lookup table i set 14500rpm as my speeds are off. The cut started and as soon as the cutter ramped in about 0.5mm of the 2.5mm set the motor bogged down like it was totally powerless and ping went £10 :(
So, back indoors, reprogrammed for about 20,000+ rpm and started again on my reserve tool, all started ok, 1st pass was flinging sizeable chips across the room, ramps down for second pass and even though i set 0.4mm holding tabs in various places, the first part broke free and fell out thus ruining that bit. Thinking the cut was too heavy i backed off the feed a bit in Mach3 and let it go, 75% of the last roughing pass and the part breaks free and takes the cutter to the bin with it. It's irrelevant but thats £25 of bits in 15 minutes, plus another sheet of 5mm Alu in the bin. :( :( Talk about pissed off!
Right, observations...
1 - Is this job actually possible?
2 - is there any point at all at running less than 100% RPM - these spindles seem to have zero power.
3 - It seems to be cutting 0.2mm below the set height - I need to tweak the Z height routine a bit, set the plate thickness a bit off to lift the tool 0.2mm
4 - How thick should holding tabs be - I set 0.4mm but clearly not enough.
5 - I set 2.5mm DOC for the roughing on a 5mm bit, go less, 1mm??
Exceedingly vexed at the moment :(
No, you need to find out why it's off by .2mm.Quote:
3 - It seems to be cutting 0.2mm below the set height - I need to tweak the Z height routine a bit, set the plate thickness a bit off to lift the tool 0.2mm
It should be right on, every time.
I will get the indicator out and re-check the steps-per setting, can't think of anything else I can do?
I use 6mm 2f carbide 45deg alum carbide bits at 12000 rpm 900 mm/ min 1.0mm DOC. Any more DOC and the motor sounds loaded and risk of gumming up is pretty high.
I also drop the feedrate manually when deep into a profile cut as the chips are harder to clear.
I often manually drop the feedrate on the first cut as the surface seems to be harder than the core. Also my ramps in and pretty slow.
I've seen others post more aggressive rates but it does not work for my machine.
My tabs are about 3mm as you are not just holding the part but stopping it vibrate on the finish pass to get the best surface finish. Means you need to cut them out with a pad saw not just push them out .
3mm wide tabs? But how thick?
I set 2mm wide x 0.4mm thick but due to my z running low for some as yet unknown reason, they came out at 0.15 mm thick.
Sawing these parts out is going to bugger the finish, is there another way?
If not then I might have to revert to sending them out for laser cutting again but i really, really do not want to have to do that.
Sorry typo
3mm high and ~12mm long
Careful filing and sanding then scouring pad gives a reasonable finish. If you want a mirror finish with no sign of tabs then you are back to fixing the part down in the middle using any holes that are available instead of using tabs.
On occasion I've also put the raw tabbed part in a vice edge up and used the machine to skim it down 0.05mm at a time and remove the last but if the tab. You can get a very good finish but you ideally need a parallel edge on the lower side to reference to sitting in the vice. But this takes time and is best for simple shapes.
Wow! 3x12mm thats a serious tab, really doubt it would go on these parts IMHO.
One idea I just had was to split the job into two overlapping parts and use solid clamps with a pause in the job to allow two new clamps to be set over the cut part and the other clamps to be removed. It would mean double the tooling changes but might work?
There are no holes for fixings internally.
I was using 1300mm/min and 2.5DOC for the 5mm single-flute tool.
Is it not possible to leave 2 or 3 decent tabs 12mm x 3mm on straight edges and remove tabs as final cut after clamping the parts?
Possibly, I'm working on it now in CAD and will post when i've got to sheet cam to see if i'm barking up the wrong tree.
Ok, lets run this up the flagpole...
This is the job - two parts. Outer line is the base metal - 5mm Aluminium, the three point down the centre are M6 screws for fixing to the bed.
Looking at it now I can pretty much see why it failed - once the last pass of the roughing cut is made down the centres there is bugger all holding the two parts to the central stub - just the centre holding tabs which were way too thin to stand up to the cut.
This is my next plan - place some full-depth tabs maybe 10mm wide where the red dots are, make all the cuts, including the finish passes, then using the 2mm finish tool add some cuts to nibble away at the tabs after maybe fixing a couple of clamps - as suggested.
Attachment 18063
Doomed to failure or possible plan ?
Onion Skin will work better has it holds all round and can be lot thinner.
To be honest Dave and no disrepect meant here and I know you have some experience with milling but think your kind of trying run before can walk with this.? By that I mean you haven't had much time using this machine so don't know it's capabiltys and your part isn't exactly new user friendly with those smaller cutters.
You may be better stepping back a little and work upto this part.
Also the Water cooled spindles above 12000rpm do have resonable amount of torque and shouldn't struggle with 5mm carbide tool while ramping only 0.5mm so are you sure you have the VFD parmaeters set correctly.?
That's the point - there is no all-round, which is why it failed. The base metal is only just over-size for the whole job, once the perimeter is roughed the only fixture it has is the middle strut and that only had the tiny tabs or possibly onion skin - just not enough meat.
No offence taken JAZZ, speak your mind ;) There is a long story with these parts, not for here but suffice to say I have customers waiting and really wanted to get them done myself instead of farming them out - this has applied some undue pressure but I think I can win still.
My experience is all manual - I'm used to throwing in a 1/2" cutter, clamping the metal down and diving in at full depth and adjusting the feed to suit as I'm twiddling the handles. The learning curve here is staggering, my presumptions were originally to use a feed and speed guide - set those parameters and have at it - this was wrong by a long-shot and I realise that now. It probably explains why 90% of the videos i have seen on youtube are all running very light cuts.
There is a slim chance that the loss of power on the spindle is connected with my odd VFD issue - maybe it really is a duff VFD after all - the new one should arrive tomorrow and i'll be fitting that before running any more tests - another good thing with a UK supplier is that help is only a call away and they are very helpful ;)
I will get that set up, check my Z axis calibration, then run some simple tests on scrap before diving in again. The new cutters will be here for the weekend and I will switch to a more softly-softly approach to feed rates as it seems most others do.
Not too softly and most do cut too slow or too shallow but it's good idea to find your feet first before gunning it. When your settled you'll be surprised how much you can push the limits with right tooling and feeds etc.Quote:
Originally Posted by Davek0974
If part has decent area to it then Double sided tape can work well if your not using cutting fluid or light amount of fluid.
Will try the DS tape, good point.
Would you agree with the "few heavy tabs and remove last" idea??
I wonder how you take so brave cuts and meanwhile try to tune your mist system....:boxing:
Why just you dont cut a 50x50 mm pieces and figure there the speeds, feeds and mist system.
Here are some tips, you could say cornerstones:
-mist system tip should be 0.8-1mm, 2-2.5 bar pressure at reservoir, mist spray length should be 80-100mm if all done correctly. when done correctly it will blow away even when 20mm bit cutting
About the cuts in aluminum. you will continue to snap bits until you don't figure what are you doing. Deep slotting is a recipe for disaster. Make slot double wide so you have space where the chips to go, or go slower.
Start from 12000rpm and ~600mm/min, slowly rise speed and look about the quality of the cut/6mm 2 flute/. But not on big pieces. Make small pieces and test all untill happy, including final slot depth test.
And better more mist than not at all
I leave 4mm thick by 10mm long tabs
Dave this what I meant when said Aluminium bed is Ok but often you'll have Spoil board on it. So here's what I would do.
Fit spoil board that can be screwed into and surface it. Then I would change the Code and move the smaller part in wards and drill holes put screws where I have black circles on your last pick.
Then onion skin the both parts with about 0.3mm. Doesn't matter the large part will not be held down one side the rest will old it.
The skin then just breaks away and quick cleanup with De-burr sorts what's left.
I do this type thing all the time in shity 1050 2mm plate and works perfectly.
Attachment 18066
Points noted Boyan, BTW the coolant is working nicely - the cutter was clear even during the heavy cuts.
Jazz, the two screws in the small cutouts - they would be fitted after the finish pass on this features?
Spoilboard - MDF?
What sort/size for facing cutters?
Yes screws with washers in cut outs after finish pass on pockets.Quote:
Originally Posted by Davek0974
MDF, ply anything that can screw into really.
Facing cutter then widest you have but with such small piece then wouldn't take long if small.
Actually to be honest dave if spoil board is resonably flat then just for this job won't even need surfacing because your only profiling. The main reason I said surface is because 0.3mm isn't much so can easily cut thru if not flat but if you want to have thicker skin then don't bother with surfacing.
Disclaimer here .!! . . . You'll need to sort that discrepency in the Z axis if your having 0.3mm Skin so don't blame if your Z isn't fettled.!
Thats task no1, I will re-check it with the dial indicator as i cant see how it was going too deep. I know the bed is 0.1mm out of parallel over ints 400mm length but this was too deep at the point i set the tool using my probe plate.Quote:
Originally Posted by JAZZCNC
My thinking is that I can set a tool, set zero height using the touch-plate, command G0 Z0.00 and run the cutter over the bed without any more than a witness mark?
The only thing i can see is the steps-per being off in Mach settings.
No2 job is fit and program the new VFD for sensors vector, might help a little, should certainly sort out that odd voltage issue on the 0-10v control, maybe even the lack of power at half speed.
No3 job is to run some tests on small scraps - i seem to have plenty now ;)
While doing all that I will be resigning my parts and maybe ordering some larger sheet stock so that it can be fixed down around the edges easier.
Getting beyond a joke now :(
Being smart ;) I programmed the new VFD at work on a test motor, all went well, nice and easy.
Just about time to fit it when i got home, booted the pc up, pressed the reset button to power up the VFD/spindle and pop goes the breaker.
Reset the mcb, try again - pop.
Ok, thinking there might be another issue here i disconnected the VFD and put a plug on it and plugged in directly - pop.
Now, this is a 32A circuit and I really can't see why a small drive like this should need a slow breaker?
Obviously no time left in the week now to replace the drive, so its a case of putting the dodgy one back now and keeping my fingers crossed.
I have emailed the supplier as they were shut by the time I came in from the shop.
Things shouldn't be this damn difficult, doing my head in now ;(
Busy time of day so, do you're breakers have an undervoltage trip? If so, something heavy starting up might be causing a dip sufficient to drop the breaker out!
Additional thought, VFD's generally default to a very fast ramp-up time, people never turn it down sometimes fixed just by changing the ramp up time.
Doubt it, just the bog-standard 32A MK mcb.